Dimensions Disappearing On Drawing

Well, I am stumped. I'm running 2017 sp4.0 with the hot fix and I getting an issue of my dimensions disappearing on my sheet metal flat pattern (only that view). I've searched the forums but it seems no one has seen this, so I know I have a setting wrong.

Basically what is going on, most of the dimensions I place on the flat pattern will disappear after a rebuild is complete. They can be placed without issue, moved as as any other day of making drawings. Do a rebuild and the work disappears.

Things I have checked:

-Layers the dimensions and view are inserted on that are active and visible.

-View sketch visibility is on. I know this would make the other views dimensions not show/show depending how this is toggled. This goes along with the rest of the items in this drop down menu.

-Used Hide/Show Annotation command, no dimensions.

-Deleted the view and reinserted the view

-Deleted the flat pattern configuration and then reinserted the view (to make Solidworks make the flat pattern) into the drawing.

-Closed restarted Solidworks

-Restarted my computer

I attached a zip file that contains the drawing and model of the part I am having the problem with.

So in the end, I am no sure what to do. This needs to be dimensioned but everything but a few will stay after the rebuild. Hopefully this is a setting I can change and I do not need to redraw the part as I will not have it much longer to redraw from...

For some reason, the suppressed 15/32 hole wizard hole is causing the problem. Delete it and the dimensions no longer disappear. In fact, if you've placed the dimensions over and over, they all come back. This might be a case of

I will admit, I cheated on the 3/4" dimension and created a line to the diameter of the arcs and hid the line since the smart dimension tool was not grabbing the arcs correctly for a outside dimension.

I will admit, I cheated on the 3/4" dimension and created a line to the diameter of the arcs and hid the line since the smart dimension tool was not grabbing the arcs correctly for a outside dimension.

Ahhh....that is a clue!

I wonder if 1 of two things is true (please check them):

1) Check to see if "True" is checked on the flat pattern view

2) Also please check that the flat pattern is square to the view (in other words, you are looking straight at the face 90 degrees from it). Is it slightly off at some angle?

A good way to check #2 above is to re-create the view and use the "Relative View" (or "Relative to Model" depending on where you select it).

Make sure that the part is in it's flat pattern config and then switch to it (after selecting Relative view from the drawing) and make the flat face the front view and some other face the right view.

Then try to re-add your dimensions and see if it has the same problem.

If that IS The problem, then there is either an issue with your template (where the "Front" view is slightly off angle) or the flat pattern is sitting skewed to the world.

Projected is selected to answer question one. To that question, the flat pattern is in its own view and not a child view of the main view. So that rules out that possibility.

The second question I have tired and it does not change. I went into the flat pattern option in the bottom of the tree and changed where the base tab unfolds from. So I changed it to the tabs that are parallel to the top plane. I inserted the view on the top view with the flat pattern config, and I still have the issue.

Projected is selected to answer question one. To that question, the flat pattern is in its own view and not a child view of the main view. So that rules out that possibility.

The second question I have tired and it does not change. I went into the flat pattern option in the bottom of the tree and changed where the base tab unfolds from. So I changed it to the tabs that are parallel to the top plane. I inserted the view on the top view with the flat pattern config, and I still have the issue.

"Projected", in that context doesn't mean that the view is projected.....it means that the dimensions are projected on the viewing plane that you are looking through when you see the view. While "true" means that it gives you the actual measurement as if you were selecting them in 3D.

Example:

As for the 2nd one, I am not totally sure that you have ruled out the possibility that your template front view is slightly off angle from the front plane. The best way to check is to use "Relative to Model" because it uses the actual geometry of the part to create the view rather than the canned Front view from the model.

For some reason, the suppressed 15/32 hole wizard hole is causing the problem. Delete it and the dimensions no longer disappear. In fact, if you've placed the dimensions over and over, they all come back. This might be a case of